A collection of libraries and tools that let the user handle OpenFOAM-data based on expressions

This file gives an overview of swak4Foam and a history of the features. It is not a canonical documentation.

This file is written in the mighty org-mode (see http://orgmode.org/) a markup/outline-mode for (X)Emacs. Using this mode it can be easily (using 3 keystrokes … it’s Emacs) to PDF or HTML to make it more readable (and add a table of contents).

Please don’t try to “beautify” it with any other text editor as this will surly mess up the markup (and keeping the file org-compatible outside of the org-mode is a pain in the neck.

The Markdown-variant README.md is only there to be displayed in a human-readable form by the web-interface to mercurial at sourceforge.net. It is generated from REAME and only updated during releases. Don’t edit it.

Bernhard Gschaider (bgschaid@ice-sf.at)

Bernhard Gschaider (bgschaid@ice-sf.at)

In alphabetical order of the surname

Martin Beaudoin

trackDictionary in simpleFunctionObjects

Martin Becker

The potentialPitzDaily-case (demonstrating a problem with groovyBC)

Oliver Borm

patchMassFlowAverage in simpleFunctionObjects

Peter Keller

sprinklerInlet-case

Martin Kroeger

mtv surface writer in simpleFunctionObjects

Andreas Otto

fixed the circulatingSplash-case

Alexey Petrov

pythonFlu-integration

Bruno Santos

• Compilation with Intel compiler and Mingw
• Rewrite of mybison and myflex to allow parallel compilation with WM_COMPPROCS
• Generation of dependencies for files that need Bison generated tab.hh files. This allows not having race conditions during parallel compilation

Hrvoje Jasak

Fixes to compile on Intel and CLang

E.David Huckaby

Add the writing of particles to writeFieldsOften

Alexey Matveichev

• release generation script.
• Automatic swakConfiguration

If anyone is forgotten: let me know

According to the commits in the mercurial-repository (and the repositories of the projects from which swak emerged) contributors are (ordered by the year of their first contribution):

• 2006-2015 Bernhard F.W. Gschaider <bgschaid@ice-sf.at>
• 2008 Hannes Kroeger (hannes@kroegeronline.net)
• 2008-2009, 2012 Martin Beaudoin, Hydro-Quebec (beaudoin.martin@ireq.ca)
• 2010 Marianne Mataln <mmataln@ice-sf>
• 2010 Oliver Borm (oli.borm@web.de)
• 2011 Alexey Petrov <alexey.petrov.nnov@gmail.com>
• 2011 Petr Vita <petr.vita@unileoben.ac.at>
• 2012-2014 Bruno Santos <wyldckat@gmail.com>
• 2013 Georg Reiss <georg.reiss@ice-sf.at>
• 2014 Hrvoje Jasak <h.jasak@wikki.co.uk>
• 2014 David Huckaby <e.david.huckaby@netl.doe.gov>
• 2015 Domink Christ <d.christ@wikki.co.uk>

See: http://openfoamwiki.net/index.php/contrib/swak4Foam

• Version 2.0 or higher of OpenFOAM and version 3.0 or higher of Foam. The OpenFOAM-dev is also supported but because this is frequently changing compilation may fail. The branch feature/port_of-dev of the development repository may work better
• the compiler generators bison and flex

  bison

  swak4Foam is known to work with bison version 2.4 and higher. Version 2.3 compiles but the plugin-functionality does not work correctly. Version 3.0 does not work

  flex

  since the introduction of the plugin functions at least a flex version of 2.5.33 is required (2.5.35 is the lowest confirmed version)

Both of these are mainstream packages (they are for instance needed to compile gcc) and should exist on every Linux distribution. Use the package manager of your distribution to install them and only if the compilation process of swak4Foam complains about too low or too high versions compile special version. This can be easily done by calling

./maintainanceScripts/compileRequirements.sh

in the directory of the sources. This will download a fitting bison version, compile it and install it in such a way that it is only used during the compilation of swak4Foam.

swak4Foam tries to keep the requirements on these as low as possible and sometimes lower versions than the ones reported may work. If they do please report so.

The version of bison can be checked with

bison -V

The version of flex with

flex -V

wmake all

at the base directory should build all the libraries and tools.

Rerun the command to make sure that there was no problem with the compilation (this should be quite fast and only report libraries being created and some administrative stuff)

Some features (currently only the Python-integration may need third party software. The paths to these packages can be configured in a file swakConfiguration (an example file swakConfiguration.example is provided. There is also a file swakConfiguration.automatic that tries to automatically determine the location of Python. It does not work on all systems and therefor is not enabled by default). If that file is not present these unconfigured features will not be compiled.

Environment variables that can be set in this file are:

SWAK_PYTHON_INCLUDE

Path to the Python.h file of the used python-installation

SWAK_PYTHON_LINK

Options to link the python-library to the library for the python-integration

SWAK_USER_PLUGINS

A list of paths separated by semicolons. These are the directories of libraries with function-plugins. They are compiled in the course of the normal swak-compilation. This makes sure that they are consistent with the swak-release in the case of an update

SWAK_COMPILE_GRAMMAR_OPTION

Additional compiler switches for the C-files generated by bison. Usually used if the default optimization switches are too aggressive and compilation takes to long (then a value like -O0 would for instance switch off all optimizations)

SWAK_COMPILE_LEXER_OPTION

Additional compiler switches for files generated by flex. For some compilers (Intel) aggressive optimization when compiling these files may cause uninitialized memory and crashes. This variable can be used to switch off the optimization (usually this fixes the problems)

SWAK_TEST_RACE_CONDITIONS

Meant to be used only by developers, for performing a verification on whether race conditions occur during parallel compilation, regarding the grammar parsers.

With older versions of 2.0.x (or 2.0 or 2.0.1) it is possible that the compilation of swakCodedFunctionObject will fail. In that case remove the last parameter to the codedFunctionObject-constructor in swakCodedFunctionObject.C (it is clearly marked by a comment)

Note: This section is very special and won’t be needed by most people

The library libswakPythonIntegration.so links against a specific version of the python library. In certain circumstances (for instance the OS of the cluster is different from the one that swak was compiled on) this python-version is not available on the target machine. While all other parts of swak will work the python-integration won’t load on the target machine. To fix this problem a workaround is provided:

The script maintainanceScripts/makeSpecialPythonLibrary.sh compiles a special version of the libswakPythonIntegration.so that is identified by an additional suffix (for instance the suffix Cluster makes a file libswakPythonIntegrationCluster.so). That script has to be run on the target system and needs 3 parameters:

1. SWAK_PYTHON_INCLUDE
2. SWAK_PYTHON_LINK
3. The suffix

For instance

./maintainanceScripts/makeSpecialPythonLibrary.sh -I/opt/local/Library/Frameworks/Python.framework/Versions/2.5/include/python2.5 "-L/opt/local/lib -lpython2.5" Version2.5

compiles a version for an old python.

To enable the python-integration in libs in controlDict both python-integrations have to be specified. One of them will fail on each machine (because the required python-library is not there), the other one will provide the python-functionObjects.

Note: the special libraries won’t be updated automatically on the target system. Doing so is the responsibility of the user.

If the libraries and utilities are considered stable and the should be available to everyone (without having to recompile them) the script copySwakFilesToSite.sh in the directory maintainanceScripts can be used to copy them to the global site-specific directories.

The script removeSwakFilesFromSite.sh in the directory maintainanceScripts removes all these files from the global directories. The removeSwakFilesFromLocal.sh does the same for the user directories (this makes sure that no self-compiled version shadows the global version (which would lead to strange results)

There is a Makefile attached. make globalinstall compiles swak4Foam and installs it into the global directories

Note: Due to the order in which library direcories are searched for with -L a global installation might break the compilation. If you don’t know what this means: don’t attempt a global installation

The command build dpkg builds a Debian/Ubuntu package for the currently enabled OpenFOAM-package. Note:

• it is assumed that the currently used OF-version was also installed by the package manager
• the dev package is built but poorly maintained

Changes in the packaging should be done in the branch debianPackaging of the Mercurial-repository and later be merged to the default-branch.

Packaging for OpenFOAM 2.x should be done in the branch debianPackaging_2.x

Note: Due to the problem described with the global installation it might be necessary to deinstall a previously installed package to successfully build a new package

Collection of Libraries

The basis of swak4Foam: the expression parsers with the logic to access the OpenFOAM data-structures.

None of the other software pieces compile without it.

Also defines a subclass to DataEntry that uses swak-expressions and a function object initSwakFunctionObject that might be used if this fails

A collection of function objects that was previously separately available at http://openfoamwiki.net/index.php/Contrib_simpleFunctionObjects.

Provides consistent output of values (on patches and fields) and more.

Implements the infamous groovyBC. A boundary condition that allows arbitrary expressions in the field-file

Function objects that have no additional requirements. Mainly used for manipulating and creating fields with expressions

addGlobalVariable

Adds a variable to a global swak-namespace. Mainly used for debugging and resolving issues where a variable is needed in a BC before it is defined.

expressionField

Create a new field from an expression

clearExpressionField

Erase a field created with expressionField

manipulateField

Modify a field in memory

createSampledSet

Create a sampled set that can be used by other swak-entities (mainly boundary conditions)

createSampledSurface

Create a sampled surface that can be used by other swak-entities (mainly boundary conditions)

swakCoded

Child of the coded-functionObject that can read and write global variables from and to swak-namespaces

Assumes that the SWAK4FOAM_SRC environment variable is set to the Libraries-directory of the swak4Foam-sources

solveLaplacianPDE

Solve the Poisson equation

\begin{equation} \frac{∂ ρ T}{∂ t} - ∇ λ ∇ T = S_expl + S_impl T \end{equation} for $T$ where $ρ$, $λ$ and $S$ can be specified

solveTransportPDE

Solve the transport equation

\begin{equation} \frac{∂ ρ T}{∂ t} + ÷(φ,T) - ∇ λ ∇ T = S_expl + S_impl T \end{equation} for $T$ where $ρ$, $λ$ and $S$ can be specified. Plus the name of the field $φ$

addForeignMeshes

this allows specifying new foreign meshes. These can be used in subsequent function-objects or other swak-expressions on internalFields

foreignMeshesFollowTime

this allows specifying a list of meshes whose time is set to the current time of the running case

Function objects based on the simpleFunctionObjects-library (which is a prerequisite for compiling it).

Evaluate expressions and output the results

These classes allow to manipulate the solution. To use these the solver has to be modified.

expressionSource

Field that is calculated from an expression. To be used as source-term or coefficient in some solver

forceEquation

force an equation to fixed values in selected locations. Has to be used after constructing the equation and before solving

These sources are based on basicSource and can be used without a modification of the solver (they are only available in the 2.x version):

SwakSetValue

sets values according to a mask or the mechanism provided by basicSource

SwakExplicitSource

Uses the calculated source term on the right hand side of the equation

SwakImplicitSource

Uses a calculated scalar-field to add an implicit source term (source is without the actual field)

Starting from OpenFOAM 2.2 this library has additional fvOptions

topoSources for cellSet and faceSet. Can be used with the cellSet and faceSet-utilities

Implements parsers for the finiteArea-stuff in 1.6-ext. Also implements groovyBC for areaField and expressionField and other function objects

Collection of boundary conditions that give standard boundary conditions the possibility to use expression for the coefficients

Contributions to this library are explicitly encouraged. Please use the Mercurial-branch groovyStandardBCs to groovyify standard boundary conditions.

Embeds a Python-interpreter.

pythonIntegrationFunctionObject

Executes Python-code at the usual execution times of functionObjects. The interpreter keeps its state

This library is only compiled if the paths to the Python-Headers are configured in the swakConfiguration-file (see above)

Function objects that allow the easy addition of lagrangian clouds to a case. No other libraries from swak4Foam are needed for this

Additional searchableSurfaces (for use in snappyHexMesh) which include boolean operations for other surfaces and coordinate transformations

Driver for functionObjects that implemented entirely in Python using the pythonFlu-library

Parser for calculating expressions on clouds of lagrangian particles

Directory with a number of libraries with function-plugins:

swakFacSchemesFunctionPlugin

functions with selectable discretization schemes for FAM (only used in 1.6-ext)

swakFvcSchemesFunctionPlugin

functions with selectable schemes for FVM

swakLocalCalculationsFunctionPlugin

calculations that are local to a cell (Minimum of the face values or so)

swakMeshQualityFunctionPlugin

calculate mesh quality criteria like orthogonality, skewness and ascpect ratio

swakRandomFunctionPlugin

different random number distributions. Currently only exponential

swakSurfacesAndSetsFunctionPlugin

calculates distances from sampledSurfaces and sampledSets and projects calculated values from these onto a volume field

swakThermoTurbFunctionPlugin

Access functions from the thermophysical model and the turbulence model in the current region. Loads the model only if necessary

swakTransportTurbFunctionPlugin

Same as above but for incompressible models

swakLagrangianCloudSourcesFunctionPlugin

Functions that get informations like source terms from clouds of particles (due to technical reasons this works only for the regular intermediate clouds)

swakVelocityFunctionPlugin

Functions that work on the flow field (currently only the local Courant-number)

swakChemistryModelFunctionPlugin

Functions that calculate chemistry properties (reaction rates etc)

swakRadiationModelFunctionPlugin

Functions that calculate properties of the radiation model

swakMeshWaveFunctionPlugin

Functions that use the MeshWave-algorithm to calculate grid-dependent properties like number of mesh layers

Because of the templating all plugin-functions have to be reinstaniated for new particle classes. The libraries in this directory

• reimplement the functions from swakLagrangianCloudSourcesFunctionPlugin
• the CloudProxy for the cloud parser

for special particle classes. These are

coalCloudAdaptor

the library libswakCoalCloudAdaptor that handels the CoalParcel-class

These libraries have to be included in the libs-entry to be able to handle these libraries

Utility that allows creation and manipulation of files with expressions

Utility like funkySetFields for areaFields (only works with 1.6-ext)

Sets any field on a boundary to a non-uniform value based on an expression.

Acts without deeper understanding of the underlying boundary condition

Utility to quickly test whether a groovyBC gives the expected results. Writes the specified fields with the applied boundary condition but doesn’t do anything else.

Can be used for other BCs as well

Evaluates expressions that are listed in a dictionary using data that is found on the disc and prints summarized data (min, max, average, sum) to the screen

Calculates the offsets-entry in the polyMesh/boundary-file according to the specification in a dictionary. Only needed if you have mapped patches and the regular uniform offset is not enough for your purposes

Utility that quickly does some quantitative analysis (minimum, maximum, average etc ) on a field on the disc (internal field but also patches, sets, zones, …)

This utility loads specified fields into memory, executes a list of user-specified function objects whose data is then passed to a python script which does the user-specified analysis.

Utility to calculate fields for a lagrangian cloud (or setting it up from scratch)

If not otherwise noted cases are prepared by a simple blockMesh-call.

Note: All the cases here are strictly for demonstration purposes and resemble nothing from the ‘real world’

Note: Due to various changes in the case syntax between OpenFOAM 2.0 and 2.2 (for instance thermophysicalProperties, wall functions etc) not all of the examples work with all OpenFOAM-installations “out of the box”. Slight adaptions may be necessary

The old groovyBC-Demos

Solver

pisoFoam

Also demonstrates

manipulateField, expressionField and clearField from the swakFunctionObjects. patchExpression from simpleSwakFunctionObjects. solveLaplacianPDE and solveTransportPDE for solving equations, pythonIntegration with calculations using numpy

Solver

solidDisplacementFoam

Solver

interDyMFoam

Solver

pimpleDyMFoam

Also demonstrates

swakExpression with surface. Due to a problem described below this currently doesn’t work

Solver

pimpleFoam

Mesh preparation

Execute the script prepare.sh in that directory (requires PyFoam: if not installed change in the boundary-file the type of the defaultFaces to wall)

Solver

pimpleFoam

Demonstrates

Delayed variables to simulate an inflow that depends on the value of the outflow

Solver

chtMultiRegionFoam

Mesh preparation

Execute the script prepare.sh in that directory

Also demonstrated

patchExpression and swakExpression from simpleSwakFunctionObjects.

Solver

interFoam

Also demonstrates

Usage of a sampledSet defined in the controlDict do determine the average filling height. Also stored variables for not switching back once the criterion is reached. Global variables defined by a function object

Solver

interFoam

Description

Winner of the swak4Foam-competition at the 6th OpenFOAM-Workshop (2011). By Peter Keller

Solver

potentialFoam

Description

Demonstrates the use of groovyB with potentialFoam (also a problem connected with that). Provided by Martin Backer

Solver

interFoam

Preparation

run pyFoamPrepareCase.py

Description

Demonstrates the use of 2-dimensional lookup tables. For the initialization as well as the boundary condition

Example dictionaries for funkyDoCalc

Example dictionary for funkySetFields

Example dictionary for funkySetBoundaryFields. Sets nonsense boundary conditions for the world famous damBreak-case

Demonstrates usage of expressionSource

Due to differences in the original interFoam-solver this doesn’t work on certain OpenFOAM-versions (most specifically 1.6-ext). The current solver works with 2.1. For older OF-versions use the sources labeled _pre2.1.

The only modifications to the original solver are found at the end of createFields.H and in UEqn.H (the added source terms).

Demonstrates usage of forceEquation

Due to differences in the original interFoam-solver this doesn’t work on certain OpenFOAM-versions (most specifically 1.6-ext). The current solver works with 2.1. For older OF-versions use the sources labeled _pre2.1.

The only modifications to the original solver are found at the end of createFields.H and in UEqn.H (the fixing of the velocities).

Slightly modified version of interFoam. Adds a source term to the momentum equation. The source term is an expression that is defined at run-time

Demonstration case for it.

Preparation

Run the script prepare.sh to prepare the case

Demonstration of the finiteArea-stuff that works with 1.6-ext

Variation of surfactantFoam that adds an expressionSource

Demonstration case

Preparation

Use blockMesh and makeFaMesh

Solver

surfactantFoam (without source term) or swakSurfactantFoam

Demonstrates

FAM-specific swakExpressions and groovyBC (as well as the expressionSource)

Cases that demonstrate swakSourceFields

Solver

rhoPimpleFoam

Mesh preparation

Execute prepareCase.sh

Demonstrates

Simple expression sources (adds a heat source to the solid)

Cases that don’t have a groovyBC

Solver

rhoPorousMRFSimpleFoam

Mesh preparation

Execute the makeMesh.sh-script in that directory. If you want to run in parallel call the decomposeMesh.sh-script with the number of processors as an argument

Demonstrates

Usage of the swakTopoSources. Compares different approaches to evaluating with the swakExpression-functionObject. Also an example dictionary that demonstrates the use of funkyDoCalc. Demonstrates “live” comparing to another case using foreign meshes

Solver

rhoPorousMRFPimpleFoam

Mesh preparation

Execute the makeMesh.sh-script in that directory. If you want to run in parallel call the decomposeMesh.sh-script with the number of processors as an argument

Demonstrates

The same as angledDuctImplicit but also the output of temporal changes

Solver

interFoam

Case preparation

run the pyFoam-utility pyFoamPrepareCase.py

Demonstrates

Usage of a sampled surface to track the interface in a VOF-simulation

Solver

interFoam

Case preparation

run the supplied script prepareCase.sh

Demonstrates

Emulate a “moving gravitation” by using the manipulateField-functionObject to recalculate gh and ghf

Demonstrates initializing a case with initial conditions that approximate the real flow.

Solver

reactingFoam

Case preparation

run the supplied script prepareCase.sh. Caution: this has to be done every time before running the case

Demonstrates

Demonstrates setting calculated initial conditions with functionObjects

Demonstrates the use of funkyWarpMesh and post-processing on bended pip geometries

Solver

simpleFoam

Case preparation

Run prepare.sh

Cases that were shown in some presentations

Solver

interFoam

Case preparation

run the prepareCase.sh-script

Description

The case described on the slides of the talk about swak4Foam at the OSCFD-conference 2012 in London

Demonstrates

Boundary conditions, function objects, global variables and delayed variables

A 2D-variant of the above case

Solver

twoPhaseEulerFoam

Case preparation

run the prepareCase.sh-script

Description

Simulate a sand-monster from the StarWars-movie “Return of the Jedi”

Demonstrates

Use of funkySetFields, groovyBC and functionObjects for lagrangian particles

solver

simpleFoam

Case preparation

run the prepareCase.sh-script

Description

Simulates two landSpeeders (as seen in the StarWars-movie “A New Hope”)

Demonstrates

Advanced searchableSurfaces (for snappyHexMesh), functionObject for passive scalar, functionObject to calculate distributions

Demonstrate the integration of Python. Mostly using PyFoam but also with pythonFlu

Solver

simpleFoam

Demonstrates

Usage of PyFoam to manipulate the fvSolution-file during the run (possible application: unphysical initial conditions cause the run to fail during startup with “normal” relaxation values)

Solver

simpleFoam

Demonstrates

Usage of the pythonFlu-integration to find the point where the recirculation behind the step ends. Also tries to plot the result using the matplotlib-library

Solver

twoPhaseEulerFoam

Demonstrates

Usage of PyFoam to read the direction of gravity and feeding it into a goovyBC via global variables

Case preparation

Just call funkySetFields -time 0

Solver

chtMultiRegionFoam

Demonstrates

Building the specification of function objects at run-time via a Python-script

Solver

simpleFoam

Demonstrates

Using a python-script to dynamically generate multiple function objects (sampled surfaces). Using stack-variables to calculate the results and write them. Using a stored stack-variable to monitor the pressure at a point and stop the run if the pressure didn’t change there for the last 50 iterations

Demonstrates working together with the coded-stuff in OpenFOAM 2.0

Examples for the functionObjects that can solve Partial Differential equations

Solver

laplacianFoam

Demonstrates

The usage of the functionObject that solves the laplacian (Poisson) equation and (hopefully) that it gets the same result as the native solver

Case preparation

Allrun-script is provided

Solver

scalarTransportFoam

Demonstrates

Solving additional transport equations

These examples test the source terms based on basicSource. They only work with OpenFOAM 2.x and all use the simpleFoam-solver

Demonstrates

Fixing the values of the velocity in a region with SwakSetValues

Demonstrates

Implementing a simple porous plug by adding the Darcy-term as a source term with SwakExplicitSource

Demonstrates

Same as pitzDailyWithExplicitPoroPlug but with an implicit source term with SwakImplicitSource

Stuff that has to do with lagrangian particles

Tests for the functionObjects that create and evolve a cloud of particles (library simpleLagrangianFunctionObjects)

Solver

replayTransientBC

Mesh preparation

prepareCase.sh-script

Demonstrates

3 clouds (kinematic, reacting, solidParticle). Loading of a thermophysical model with a functionObject. Plugin functions for information about the clouds

Solver

rhoPimpleFoam

Demonstrates

Thermo-cloud. Functions for lagrangian particles

Solver

icoFoam

Demonstrates

Simplest way to add particles to a case

Testing the cloud-parser for lagrangiant particles

Solver

reactingParcelFoam

Demonstrates

Adding evaluations on the cloud to a regular case

Variation of the tutorial case

Solver

coalChemistryFoam

Demonstrates

creating new clouds with funkySetLagrangianField and evaluations on clouds during the simulation

Mesh preparation

run the prepareCase.sh script to set up the mesh and the fields

Examples for the use of the simpleSearchableSurfaces-library.

Solver

simpleFoam (alternatively use the caseRun.sh-script)

Case preparation

Script caseSetup.sh is provided

Demonstrates

Using the same STL-file more than once in a case by applying coordinate transformations. Note: the physics of this case are more than questionable as the frame of reference for both motorbikes is wrong

Solver

interFoam

Case preparation

Script caseSetup.sh is provided

Demonstrates

Boolean operations on STL-files

Solver

electrostaticFoam

Case preparation

Script caseSetup.sh is provided

Demonstrates

Boolean operations with regular surfaces

Physics of the case not as expected (charge-distribution)

Demonstrates the use of function objects that change the numerics during the run

The regular simpleFoam-tutorial. Modified so that it switches to higher relaxation factors during the run

Simple test cases for specific features. The names of the directories should give you a hint what is tested there. Most of them don’t need a real solver but replayTransientBC or scalarTransportFoam.

Note: for some features these cases are the only example there is. Sorry

Testing of different seeds for the rand-function. Also tests the randFixed-function

These are cases provided by users to demonstrate bugs. Not maintained nor documented and may be removed at any time

Undocumented scripts used for maintaining swak4Foam. If you don’t understand them, don’t use them

Additional documentation. Most written in org-mode

Current contents:

swak4FoamReference

Reference manual of swak4Foam. Especially concepts like expression syntax and parameters

Scripts and configuration to test for a release in a virtual machine using vagrant. Also to be used for packaging

The preferred place for bug reports is http://sourceforge.net/apps/mantisbt/openfoam-extend/search.php?project_id=10&sticky_issues=on&sortby=last_updated&dir=DESC&hide_status_id=90

A sourceforge-account is required for reporting

Please always report the FOAM-version you use. As OpenFOAM-dev is a moving target only bug-reports that add fixes are handled for this.

If you’re reporting a bug about the compilation please run Allwmake twice and only report the messages from the second run. This makes analyzing the log easier as only the unsuccessful commands will be reported.

If the problem seems to be a missing library rerun the compilation to make sure that there wasn’t a problem with that.

Contributions to to swak4Foam are most welcome. If you want to contribute clone the Mercurial archive of the sources

hg clone http://openfoam-extend.hg.sourceforge.net:8000/hgroot/openfoam-extend/swak4Foam

Change to the branch that you want to improve (usually default) and create a new branch

hg branch <branchName>

where <branchname> is an easily identifiable name that makes the purpose of the branch clear (for instance hotfix/WrongRandomFunction or feature/HyperbolicFunctions). Don’t work on the default branch or any other branches that are not “yours”. Such contributions will not be merged

Once development on the branch is finished export the relevant changesets with

hg export <nodeID>

(nodeID being the ids of “your” changesets) and send them to the maintainer (or attach them to a bug report on Manits). The changes will be reviewed and merged into the default branch (do not attempt to do this yourself). Patches generated with hg export make sure that all changes are attributed to the original developer (you).

An alternative would be the bundle command. Just do

hg bundle <bundlefile>

and then send the bundlefile. This will include all commits that are not in the upstream repository and will allow similar inclusion in the upstream as export.

Once you have proven by successfully submitting changesets via hg export you can ask for write access to the mercurial repository.

Only if you got through Mercurial it can be ensured that your contribution is recognized (if you want to stay anonymous send patches).

These topics may be “new” for the average OF-developer:

Mercurial

A short tutorial on this can be found at http://mercurial.selenic.com/guide/. If you already know git the http://mercurial.selenic.com/wiki/GitConcepts may be enough for you

bison/flex

This pair of compiler generator tools generate the parsers for the expressions. Google for a tutorial that looks promising to you.

For a short example that shows how a new function was added to two parsers have a look at this changeset that added the cpu()-function to the field and the the patch-parser (usually you’ll have to write a new method for the driver too):

hg diff -c 8604e865cce6

Currently the main branches are:

default

The main branch. This is the brancht that the general public will receive. It compiles under OpenFOAM 2.0 and higher

debianPackaging

Branch for generating new Debian-packages of swak4Foam. If somebody wants to “inherit” this: contact the maintainer

develop

Actual development branch

As an experimental feature distributed bug-tracking was introduced using the Artemis-extension for Mercurial (see http://hg.mrzv.org/Artemis/). An up-to-date version can be installed by

hg clone http://hg.mrzv.org/Artemis/

somewhere and installing the plugin by editing .hgrc.

This is not the official bug-tracker for swak4Foam. It is used for keeping track of new features that are to be introduced to swak4Foam and may be discontinued if the experiment proves to be unsuccessful.

The repository comes with a .hgflow-file that is set for the hgflow-extension found at https://bitbucket.org/yujiewu/hgflow/wiki/Home (there are multiple branches of this extension. This seems to be the most up-to date and still under active development)

In the future this repository will try to stick to the model described in http://nvie.com/posts/a-successful-git-branching-model/

swak4Foam is free software; you can redistribute it and/or modify it under the terms of the GNU General Public License as published by the Free Software Foundation; either version 2 of the License, or (at your option) any later version. See the file COPYING in this directory, for a description of the GNU General Public License terms under which you can copy the files.

The following list is not complete. If the Artemis extension (see above) is installed then

hg ilist

gives a more up-to-date list

It seems that with moving meshes sampledSurfaces don’t get updated. This seems to be a problem with OpenFOAM itself (the regular surfaces-functionObject doesn’t get updated. This is currently investigated

Apart from patches and internal fields the support for interpolation from cells to faces (and vice versa) is incomplete as well as point fields (although they are supported in the grammar)

This is especially evident for the funkyDoCalc-example

Not really bugs, but stuff that bugs me

This is necessary because of bison. Investigate possibilities to replace these by tmp and autoPtr

valgrind reports some lost memory for stuff that is not directly allocated by swak4Foam (in OpenFOAM-sources)

Will investigate. Relevant places are marked by comments in the code. Also the construction of sampledSet seems to loose memory

Currenly problematice parts seem to be:

• update and magSf-calculation of SampledSurface (marked in SampledSurfaceExpressionDriver.C)
• Python interpreter (but no calls in swak were found in the stack-trace that could be responsible)

Before OpenFOAM 2.1 the inner product of two symmetric tensors was a symmetric tensor. Since 2.1 it is a general tensor. As the general treatment in the grammar would be confusing currently the this product was removed from the grammar and therefor will not be correctly parsed

The same problem that was mentioned in https://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=130 is also true for subsets. But as the interpolation is not implemented for most subsets this will be postponed

The tab-completion does not work except for up-to-date versions of IPython. This seems to be a problem with the readline-library inside an embedded Python. Low priority

If the commsType is set to blocking then the MPI-communications of groovyBC cause problems in MPI and a fatal error.

Currently the only workaround is to edit $WM_PROJECT_DIR/etc/controlDict so that a different commsType is used (nonBlocking or scheduled)

Older Foam-versions had the problem that when the surface changes the size then certain values (especially the mag are not properly recalculated).

This causes this bug: https://sourceforge.net/p/openfoam-extend/ticketsswak4foam/231/

The bug can not be fixed in swak4Foam but has to be fixed in the Foam-Distro

First Release

New release Most important changes

Now expressions for the field on a sampled surface can be evaluated. All sampledSurfaces offered by OpenFOAM now can be used

The variables entry (most notably used in groovyBC and swakExpression) now can be a list of strings. This allows some kind of “formatting” (one expression per line) and should improve readability

These can copy the libraries and utilities to the global installation (for those who think that the swak4Foam-stuff is stable enough and want to ‘bless’ all users at their site with it). Note that any local installation still takes precedence (because $FOAM_USER_APPBIN is before $FOAM_APPBIN in the $PATH

This allows the inclusion of other parsers with the regular swak4Foam parsers and include them seamlessly with the variables-mechanism for ‘externals’ (in other words: you can add your own parser in a separate library without having to change anything about the overall swak4Foam, but it behaves as if it was part of it)

Now there is support for the finiteArea-library found in 1.6-dev. The support is found in a separate library swakFiniteArea. It has

• a parser faField for areaFields
• a parser faPatch for patches of areaFields
• a variant of groovyBC for these patches
• a computed source faExpressionSource
• Function-object-variants for areaFields: clearExpression, expressionField and manipulateField. These work the same as their volField-counterparts

See https://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=49

See https://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=44

New features and changes are (this list is not complete):

Like funkySetFields for finiteArea. Also writes out a volume field for easier post-processing

Makes it easier to use the groovyBC-machinery for other boundary conditions. Two standard boundary conditions were groovified. Others may follow

If no simpleFunctionObjects are present they can be downloaded by a script. Also scripts to handle global installations of swak4Foam

A class to force equations to certain values according to expressions

Utility does calculations on saved results and outputs single numbers (min, max, sum, average) to the terminal. Can be used for reporting or validity checks

Crude packaging for Debian

A single-argument function can be specified as a piecewise linear function. Basically works like timelines but the argument can be something else (not only the time)

Variables that store their values between time-steps. Applications are statistics or switches

Sampled sets can now also be used as en entity on which calculation is possible.

This is the first release that officially supports OpenFOAM 2.0

Also it is the first release that incorporates the simpleFunctionObjects-library

• These two functions now can receive an integer seed that determines the pseudo-randooom sequence generated by these functions
• Two functions randFixed and randNormalFixed were added. While the usual rand functions generate a different result at every time-steps for these functions the pseudo-random sequence is determined only by the seed (not by the timestep)

Take the bigger/smaller of two fields. Helps avoid ?:-operations

Application: If the results of the calculation are only needed in ParaView

• Use autoPtr for sets
• Update sets that change in memory or on disc

Fixed by Petr Vita

Calculated boundaries were $0$ and caused a division by zero

• Packaging information for the currently used OF-version is generated (allows a separate swak-package for every OF-version
• Submission to launchpad added

Now install to FOAM_SITE_APPBIN/LIBBIN

Uses the usual -region-option. Looks for a separate dictionary in the system-directory of that region

This can be switched on using the allowFunctionObjects-option

Allows the execution of Python-Code in a functionObject

This feature is still experimental and the organization of the libraries is subject to change

It is now possible to define variables that are ‘global’: They can be read in any entity.

Currently these variables can only be uniform.

To access global variables the specification-dictionary has to have a wordList named globalScopes. The scopes are searched in that order for the names of global variables. Having scopes allows some kind of separation of the variables

Adds a functionObject swakCoded that extends the coded-functionObject to read and write global variables

Added a boundary condition than allows to only fix the values. This should help to avoid problems with cases that don’t like mixed (on which the regular groovyBC is based)

Two function objects that solve Partial Differential Equations during a run have been added:

• one that solves a laplacian (Poisson) equation
• one that solves the transport equation for a scalar

The relevant coefficients (including explicit and implicit source terms) can be specified using expressions

Added a script that takes the current sources, copies them into the appropriate places of a OpenFOAM-installation and slightly rewrites them to compile in this place. What happens then (committing them into the repository or just plain compilation) is up to the maintainer

As many parts of swak4Foam depend on it the simpleFunctionObjects have now been absorbed into swak4Foam. They can still be compiled on their own

If a variable is defined and the patch which it is defined on doesn’t have any faces the variable is reported on that processor as not existing and the whole run fails

Fixed according to a suggestion by Andreas Otto. Now runs again (used to crash some time-steps into the beginning)

The Allwmake-script now checks for the correct bison-version (and the existence of bison) and fails if it doesn’t seem to be the right one

To allow distinguishing different OF-versions as discussed in the bug report http://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=114 the Allwmake-script now generates a header file foamVersion4swak.H that defines the symbols FOAM_VERSION4SWAK_MAJOR, FOAM_VERSION4SWAK_MINOR and FOAM_VERSION4SWAK_PATCH

• now can also produce surfaceFields
• full support of tensor, symmTensor and sphericalTensor

• now can also produce edgeFields

No support for tensors yet

If necessary (for instance swakExpression-functionObject) the storedVariables are written to disc (into a subdirectory swak4Foam of the timestep) and are reread at the start. This allows consistent restarts (for instance if a flow was summed using the variable) if the expressions stay the same.

Data files can now be written without brackets but each component on its own. The number of entries in the header is not adjusted

For drivers that don’t have access to a fvMesh a default mesh exists. This default mesh is defined by the first fvMesh that is used during the construction of any driver.

Definition of the default mesh can be forced using the initSwakFunctionObject (see the test case flowRateAngledDuct)

Due to the refactoring of the FieldDriver now phi can be specified by a general expression (instead of ‘only’ a field-name)

Can write surfaceVector and surfaceScalar-Fields. Condition has to be consistent

expressionField and manipulateField now can create or modify surfaceFields

funkySetFields and the function objects expressionField and manipulateField now also work with the three tensor-types

If the expression evaluates to a surfaceField then this is used as a flag whether or not the face is in the faceSet. If the expression evaluates to a volScalarField then the old semantic applies (faces are in the set if one cell is true and the other is false).

This only works for internal faces

If there is an entry globalVariables then this dictionary is used to set the variables

Calculates variables and then pushes them to a global namespace

New option added that generates a phi field with value $0$ to keep boundary conditions like inletOutlet happy

The functionObject dumpSwakExpression dumps the complete results of a swakExpression to file at each timestep. This produces huge files and is therefor not endorsed

Add the options allowFunctionObjects and addDummyPhi to execute functionObjects and add a phi-field (for fields that require these)

Based on the directionMixed boundary condition this allows to set a boundary condition as a Dirichlet-condition only in certain directions while in the other directions it is a gradient-condition

Boundary condition that imposes a jump in the value on a cyclic boundary condition pair (based on jumpCyclic). Only works for scalar values

Setting the option outputFileMode to csv writes CSV-files. The option-value foam is the default (old style). The option-value raw writes the values delimited by spaces (no brackets for vectors and tensors)

If a submesh is not yet in memory and the option searchOnDisc is set, the mesh is automatically read into memory and kept there

The simpleFunctionObjects-library now has a number of functionObjects that allow the conditional execution of a list of function objects.

These are

executeIfExecutableFits

if the name of the executable fits a regular expression the function objects are executed

executeIfObjectExists

if a named object exists (or alternatively: doesn’t exist) in the registry execute the function objects. Type checking also implemented

executeIfEnvironmentVariable

execute if an environment variable satisfies a certain condition (exists, doesn’t exist, fits a regular expression)

executeIfFunctionObjectPresent

execute if a specific functionObject is present. This can help prevent failures if a functionObject is missing for technical reasons

In addition the simpleSwakFunctionObjects-library has

executeIfSwakObject

Evaluates a logical swak-expression. The results are either accumulated using logical or (if one value is true the result will be true) or logical and (all values have to be true)

The pythonIntegration-library has

executeIfPython

Evaluates a Python-code-snipplet that returns a value. If this value is “true” in Pythons standards then the functionObjects are executed

simpleFunctionObjects has an additional function object that reads the direction of gravitation. The purpose is to assist boundary conditions like buoyantPressure that rely on it to work. Best used together with conditional function objects (“If g is missing ….”)

Solve transport and laplacian equation

This is defined in the swak4FoamParsers-library. The class needs a default mesh defined to construct the driver. Definition of the default mesh (if no other driver was constructed in some function-object or by a groovyBC) can be forced using the initSwakFunctionObject (see the test case flowRateAngledDuct)

Similar to the surfaceFields in funkySetFields

The Utilities failed with the Intel-compiler. Compilation now falls back to good old g++

Because the tokens were not defined in the flex-files getting tensor components with tensor.xx did not work. Fixed

Because surfaceFields know no zeroGradient the template makeConstant did not work

Change so that the field gets temporarily loaded to calculate the gradient on the patch. Same for internalField and neighbourField

The reason is that groovyBC usually doesn’t get evaluated during construction. The reason is that it is hard to tell whether all required fields are already in memory. The current fix is a workaround: setting evaluateDuringConstruction to true forces the BC to be evaluated during construction

Extra evaluation of boundary condition that should fix the problem with calculated patches causes funkySetFields to fail with stock boundary conditions if not all fields are present in memory

This boundary condition will be removed in future releases because the base class now supports the more general DataEntry-class for which a swak-subclass exists

To distinguish the output of various instances of functionObjects from the simpleFunctionObjects-library in multi-region cases the screen-output is prefixed with the region name. For the default region nothing changes. Directory names stay the same as they are unambiguous anyway (they contain the name of the functionObject)

For fields (not expressions!) the value at a previous timestep can be gotten via oldTime(field) if that information exists (also for funkySetFields if the corresponding file field_0 exists.

For fields that support it (basically volume-fields) there is also a ddt-operator that calculates the explicit time-derivative (if information about the last timestep exists)

Currently implemented for

internalFields

oldTime and ddt

patch

only oldTime

cellSet,cellZone

only oldTime

sampledSurface,sampledSet

only oldTime

faceSet,faceZone

oldTime

internalFaFields

oldTime and ddt

faPatch

only oldTime

If there is no old time value stored and in the parser dictionary the parameter prevIterIsOldTime is set, then the previous iteration value is used as the old time.

Based on the directionMixed boundary condition this allows to set a boundary condition as a Dirichlet-condition only in certain directions while in the other directions it is a gradient-condition

Note: this should have been in the last release but was forgotten to merge into the default branch

Boundary condition that imposes a jump in the value on a cyclic boundary condition pair (based on jumpCyclic). Only works for scalar values

Note: this should have been in the last release but was forgotten to merge into the default branch

The functions minPosition and maxPosition return the position of the minimum or the maximum of a scalar field

This is implemented for all field types

Now can read and generate pointFields.

Detailed features (apart from the standard symbols) are:

• Function point generates a constant pointScalarField
• Function pts() returns a pointVectorField with the point positions
• Functions pzone and pset generate logical fields according to existing pointZones or pointSets
• Functions interpolateToCell and interpolateToPoint interpolate from pointFields to volFields and from volFields to pointFields

Utilities and functionObjects affected by this are

• funkySetFields
• new topoSource expressionToPoint
• expressionField and manipulateField now can deal with pointFields

The faField-parser now supports tensors, symmetric tensors and spherical tensors.

Not all operators are supported because the are not instantiated in 1.6-ext

These variables are added in the namespace to ease the writing of Python-code whose output is consistent with OF

timeName

Name of the current time as a string. Allows the construction of directory names

outputTime

Boolean that indicates whether this is a timestep where OpenFOAM will write output

The missing operators from the fvc-namespace have been added to the Field-parser. These are

d2dt2

for all volumeFields

flux

for all volumFields. Needs a surfaceField as a first argument

meshPhi

for volume-vector-fields. Optional with a scalar-field that acts as the density as the first argument. Only works in the context of a solver with a dynamic mesh and hasn’t been tested yet

The only missing operators from the fvc-namespace are volumeIntegrate=/=domainIntegrate. These have been omitted as they are trivial to implement using other functions

Thanks to patches supplied by Bruno Santos (see http://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=105) compilation of the libraries is now possible in parallel

Releases up to now got a version number. Utilities now report the version number. This should make it easier to find out whether problems are due to an old version

Still looking for a way to do that for the libraries (so that they will report it if dynamically loaded)

make dpkg now genrates also a valid package if the current OpenFOAM-installation is not installed using the dpkg.

For parallel runs the content of the caseDir-variable changed and a few variables have been added

caseDir

in parallel runs now points to the FOAM_CASE instead of the processor subdirectory

systemDir

points to the global system-directory

constantDir

points to the global constant-directory

procDir

in parallel runs points to the processor-subdirectory of the current CPU

meshDir

The mesh data (of the current processor in parallel runs)

timeDir

Directory where data would be written to at the current time (processor dependent)

In parallel runs the user must set the isParallelized to true if the parallelMasterOnly is set to false.

With that he indicates that in his opinion the Python-code has no bad side-effects in parallel runs and that he doesn’t blame swak4Foam if anyting bad happens

As reported in https://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=119 due to a change the way the PISO-loop is treated the interFoamWithSources and interFoamWithFixed don’t compile with 2.1 anymore.

To avoid #ifdef in the solver sources there is now a separate set of sources (labeled pre2.1) for older versions. The regular sources work with 2.1 (and hopefully the following)

Function-objects only work with the while(runTime.loop())-construct in 2.1. The utility now uses this.

Bug reported: http://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=124

An expression like 2*U did not work for the field U. Reason was that the registry already held an object called U (the dictionary representation of the field) and therefor refused to load/register another U.

Has been fixed by de-registering the dictionary U immediately after loading.

The gradient for a vector field (result: a tensor field) was not calculated. It is now part of the grammar

tr, inv and det were not working for some tensort types in 1.6-ext. The parser now fails if such a combination is used. Works OK for other OF-versions

Also introduced a workaround for certain operators not being properly defined for pointFields (by using the internal fields)

These symbols could not be used as field names because they were used for the components of vectors and tensors

Now these names are only used if the .-operator asks for a component. This is implemented for these parsers

• FieldValues
• PatchValues
• SubsetValues (all Zones, sets and samples)
• finiteArea-Parsers: faPatch and faField

All parsers except the field-parser were missing the access to tensor components in the grammar

As mentioned in https://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=130 it was not possible to construct a point-vector field using vector(toPoint(1),toPoint(1),toPoint(1)). Same for tensors

The error message in funkySetFields that was issued when a field is supposed to be created was not very helpful (something about the field currently being an IOobject)

This function was reported missing on the message board

The composed objects got their size from the current parser, not the components. This resulted in a segmentation-fault for pointFields

Preprocessor symbol linux unknown. Replaced with __linux__

Now handles bad or non-existent filenames for dictionaries to track

Fix provided by Martin Beaudoin

This version is needed for the reentrant parsers. 2.5.33 may work but is untested. Version 2.5.4 which is on some old systems definitely does not work

Version 2.3 compiles but there is an offset-problem with the locations that breaks the Plugin-functionality

Mac-users will have to install bison from another source (for instance MacPorts)

On Ubuntu /bin/sh is something else and the scripts fail. Hardcode to /bin/bash

This script (which was removed long ago) was still referenced in the Makefile.

grad and other operators from fvc added dimensions to values that were supposed to be dimensionless. This has been fixed

Due to a typo the constructed condition field was too short for surface-fields (too long for volume-fields, but that didn’t matter)

The field-driver created patch fields there as calcuated when zeroGradient would have been more appropriate

A SortableList was used which meant that the vector with the flip values was not in the correct order

This problem was due to a non-special treatment of faces on the boundary. Fixed (for faceZone as well).

Also boundary faces are now honored in expressionToFace if the expression is a surface-field (for the volume-field logic boundary faces will never work)

The reason was that during construction refGradient, refValue etc were not read correctly (if present).

This is now fixed in groovyBC and the other BCs (groovyBC for pointFields and groovyBCDirection)

The Lexer correctly identified the variable but the getField method did not know how to get it.

Fixed

If no condition was evaluated the utility generated a pseudo-field of the wrong length

For some operations in the Field-driver the calculated-patches had the value $0$ instead of the number of the next cell. This caused certain calculations to fail (give $0$)

The FaField-driver did no fixing of the calculated-patches at all.

This is fixed

Reported in http://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=150

Added the sqr at the right place to the grammars. Also some other missing tensor operations (dev and symm).

Patch fields were not copied any no correctBoundaryField was called for technical reasons.

Fix: values copied by hand

Introduced a preprocessor symbol that allows using sortedToc on newer versions

This was due to a strange () (still don’t know what happened there)

The strings of parsed IDs were not properly deleted. Funnily this was done correctly in the Patch and the Subset-driver. Also for timelines-

Also fixed a leak with the labels of plugin-functions that was present with all drivers

Reported by Oliver Krueger that on systems where /bin/sh is not a bash anymore (newer Ubuntu and SuSE) the sourcing of theFiles.sh doesn’t work anymore.

Fixed and moved all the files to the maintainanceScripts-folder

Added. Diag had to be reprogrammed as it is not implemented for fields (probably for performance reasons).

Also some tensor operators were missing (probably lost during copy/paste)

Reported in https://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=153

Fixed by removing all file pointers if the number of patches changes

Spaces in the list of variables made the reading fail because words can’t contain spaces. For instance

"var =T*2;"

Now all the spaces are removed before assigning to variables. This will also remove spaces on the “inside” thus making

"v ar =T*2;"

the same as the above expression. But it is unlikely that the call will be used in this way

These valid div-operations were missing from the grammar:

• Divergence of a volume-tensor (all three kinds) producing a vector
• Divergence of a surface-tensor (all three kinds) producing a volume-tensor

Fields created by that function object were written with the value from the timestep before because the regular write occurs before the execution of the function objects.

Fixed

Now an initial value is required (instead of the default empty string which caused parser failure)

Reason is that during the calculation of the variables dimensions are checked.

Now the functionObject switches the checking off. But a more general solution is desirable

The functionObject does not write (and calculate) the field at the last timestep.

Fixed with an one-liner

Reason was an uninitialized valueFraction which sometimes has values that cause a floating point exception. Fixed

Because size() was equal to the expected size on some processors. Not on all. Now the branch is taken if the size is equal on all processors

Fields were not written after the boundary condition was updated. Now they are

The topology operators expressionToCell, expressionToFace and expressionToPoint now support variables and the other supporting keywords if being constructed with a dictionary (for instance from the topoSet-utility)

Usually the manipulated version of the fields is not written as the manipulation happens after writing. The option writeManipulated enforces writing.

Writing is not the default behavior to avoid side-effects

The function onPatch(name) returns a surface-field that is $1$ on all faces that belong to patch name.

The function internalFace() is $1$ on all internal faces and $0$ on all patches

Now the second argument to the pow-function can be a non-constant

The expression A.T() transposes the tensor A (for symmetrical and spherical tensors it leaves them untouched)

If no field I is defined then this is used as the unit-tensor

The unary operator * calculates for tensors and symmetrical tensors the hodge dual

The optional entry useFunctionObjects switches on the execution of function objects during the calculation

The optional entry addDummyPhi creates a phi-field

The dimensions-entry is now read at the same time the variables are read (this should work for all programs/functionObjects where the parser is not constructed using a dictionary but the dictionary is later searched for the variables-entry)

This allows easy extension of the functionality of swak4Foam without modifying the grammar files.

The way it works is that new functions are added to a runtime-selection table. If the grammar can not resolve a symbol as a built-in function or a field (but only then) it looks up the name in this table and evaluates the function. Parameters are parsed separately and can be:

primitive data types

integer, float, string and word

swak-expression

an expression parsed by one of the swak-parsers. The type of this expression does not necessarily have to be the same as the one of the ‘main’ expression.

The first time a plugin function is searched swak4Foam prints a list of all the available functions of this type. Information included is the return type and the types of the parameters (these include the parser used, the expected type and a parameter name).

Libraries with plugin-functions are added via the libs-entry in the system/controlDict

A number of plugin-libraries are already included covering these topics:

• Evaluation of functions of the turbulence, transport or thermo model
• Different random number distributions
• Functions to “project” sampledSets and sampledSurfaces onto a volume-field
• Execute explicit discretization functions (like grad) but select the used scheme in the function instead of using the value from fvSchemes
• Calculations of the mesh quality (same way checkMesh does) and return as fields
• Do calculations locally on a cell (like the maximum on its faces)
• Get the source fields and other properties from lagrangian clouds based on the basic intermediate cloud classes (Kinematic, Thermo, Reacting, ReactingMultiphase)

It has been tried to make the names unique instead of short. Usually function names from one library are prefixed with the same short string.

The new dynamicFunctionObjectListProxy in the simpleFunctionObjects can generate a functionObjectList from a string and execute them during the run like regular function-objects.

The string is provided by a special class (the so called dictionaryProvider). Current implementations for the provider are:

fromFileDictionaryProvider

reads the text from a dictionary file

stdoutFromCommandProvider

executes a program and takes the standard output as the dictionary text

stdoutFromPythonScriptProvider

executes a python-script and takes the stdout as the dictionary text

The string must be in the format o a regular OpenFOAM-dictionary with an entry functions from which the functionObjects are generated

This FO in the simpleFunctionObjects reads a number of fields and updates their boundary conditions at every timestep.

Main purpose is to let groovyBC do calculations and use the results for post-processing purposes

Does not support surface-fields as these don’t have a correctBoundaryConditions-method.

Example of the usage in the angledDuctImplicit-case (the results are of limited value because of the temperature boundary condition)

Three source terms were added. These source terms are in the swakSourceFields-library and can be used with solvers that use the sourcesProperties-dictionary. The sources are

SwakSetValue

sets values according to a mask or the mechanism provided by basicSource

SwakExplicitSource

Uses the calculated source term on the right hand side of the equation

SwakImplicitSource

Uses a calculated scalar-field to add an implicit source term (source is without the actual field)

These fields are only implemented in the 2.x-version of swak because the interface of basicSource is very different in 1.7 and a backport was unnecessary

simpleFunctionObjects now has a function object writeAndEndFieldRange that stops a run (and writes the last time) if a field is outside a specified range.

A similar function object writeAndEndSwakExpression is in the simpleSwakFunctionObjects that stops if a swak-expression evaluates to true. writeAndEndPython does the same in pythonIntegration.

Note: after the run is written one more timestep is calculated (this seems to be due to the fact that FOs are calculated at the start of a timestep). Also there are issues if the next timestep is a scheduled write-time (this only seem to be an issue with 1.7.x. It all works fine on 2.1.x)

New function objects in the simpleFunctionObjects allow the loading of such models for solvers/utilities that don’t have such models but where some functionObject (for instance) needs such a model to be in memory

Added as part of the simpleFunctionObjects some functionObjects that create a cloud of particles and evolve them at every timestep.

The appropriate fields needed by every cloud have to be present (either supplied by the solver or via a functionObject)

This function objects allows the manipulation of patch fields like manipulateField allows the manipulation of the internal field. Only use if desperate

If a variable is declared in the delayedVariables-list then its behavior changes: when a value is assigned to that variable then the value is not immediately used but after the time specified in delay. Values are stored at intervals storeInterval and interpolated linearly. If no stored data is available then the value of the expression startupValue is used.

This feature allows the modeling of boundary conditions that react with a delay to flow conditions

To satisfy the requirements of certain boundary conditions funkySetFields now allows the preloading of fields. This is only available in dictionary mode with the preloadFields-entry (for each entry in the expressions-list separately)

The environment variable SWAK4FOAM_SRC is needed for the swakCoded-functionObject. The Allwmake-script now checks whether this variable exists and prints a message with the correct value if it doesn’t. It also checks whether the value is correct and warns if it isn’t

The links to mybison and myflex are missing when the sources are downloaded as a tarball. The Allwmake-script now creates these links if they are missing

Sources of the parsers have been completely reformatted to make them more readable and maintainable

Make the directory a little bit cleaner

To avoid clashes with other similar efforts (not that I know of any) the library libpythonIntegration.so has been renamed to libswakPythonIntegration.so.

Usually only the libs-entry in the controlDict has to be changed (if the library is used at all). Names of the function objects stay the same

Now the outputControl-entry is honored. If set wrong the field is no longer calculated/manipulated at every time-step

Branch only compiled on 2.1, but not on 2.0 due to changes in the OpenFOAM-API

Fix provided by Bruno Santos

If no refValue is given during construction then a value of $0$ is assumed for this and during a preliminary update the value is reset to this value.

Fixed by using the value as the refValue if no refValue is specified

The error message occured much later when a tmp tried to copy a NULL-pointer and was not obvious at all for the general user. Fixed

1.6-ext does not consider the product of two symmetrical tensors to be symmetrical. Fixed

Change in the interface of the ExpressionResult-class broke the access of global variables from a Python-functionObject. Fixed

This didn’t influence the compilation (as there is already a current version file there) but confused people.

Face and point fields did not propagate the information correctly and were treated as non-uniform volume fields of the wrong size. This should now be fixed

The reason was that the patches of the divisor had a value of zero. This has been fixed by only dividing the internalFields(). Same for pointFields.

This kind of patch was not identified as something that could have the value fixed

The definition of the operator lessOp clashed with another definition. Renamed.

Fix provided by Bruno Santos

expressionFields were calculated at every time-step, even if the computational cost was high. Now if outputControl is outputTime the field is only calculated if it is going to be written

Seems like this one was overlooked because gcc is more tolerant towards stupidity.

Reported by Edo Frederix

On the slides the case files were promised

It is now possible for expression on internalFields to access fields from different cases. These fields are always read from disk when being accessed for the first time and stay cached in memory until the time is changed. The data is interpolated to the current mesh with the meshToMesh-class (which is the workhorse of the mapFields-utility)

The meshes are stored in a repository and are accessed via a name. If for instance the mesh is known under the name otherMesh then in an expression the term otherMesh(T) is the field T from that other mesh at the specified time interpolated to the current mesh.

Certain function objects and parser instances allow specifying foreign meshes in a subdictionary foreignMeshes.

This is the long asked for feature to “get non-uniform values from other patches”. It only works if the patches are specified as mapped (or directMapped for 1.x). Therefor a patch can only access one other patch with this.

On a mapped patch mapped(T) gets field T from whatever this patch maps from (other patch, cells, faces). mappedInternal(T) gets the values from the internal cells on the other patch (this only works for patches).

On a mapped patch an external variable expression for patches now changes its meaning: if other is the patch that the current patch maps from (and only then) then var{patch'other}=expr evaluates expr on the other patch and then maps the values to the current patch (var may be non-uniform). In all other circumstances var will get a uniform value which is derived from whatever expr evaluates to.

To allow non-uniform offsets in the specification of mapped patches in polyMesh/boundary a utility calcNonUniformOffsetsForMapped was developed.

The framework for function objects that manipulate the runTime were added. The concrete implementations are

setDeltaTByTimeline

set the timestep from a data file

setDeltaTWithPython

set the timestep by evaluating a Python-snipplet that should return a floating point number

setEndTimeWithPython

set the end time from the evaluation of a Python-snipplet

The library libswakChemistryModelFunctionPlugin adds the possibility to calculate properties of the chemistry like reaction rates, chemical timescale and released energy.

Currently only implemented for psiChemistryModel

If there is no chemistry model in memory it will be loaded and the reaction rates are calculated.

There is a function psiChem_updateChemistry that forces the chemistry to be recalculated with a specified timestep. For technical reasons this returns a scalar field with the value $0$. So an expression like psiChem_updateChemistry(0.0001)+psiChem_RR(CH4) calculates the reaction rate assuming that the timestep is $0.0001$.

Two additional functions that sum up all the reaction rates (this should be $0$) and sum up only positive reaction rates (giving an impression on what is going on)

The library libswakRadiationModelFunctionPlugin adds the possibility to calculate properties of the radiation like parts of the source terms Rp and Ru and the current radiation source

If there is no radiation model in memory it will be loaded and the reaction rates are calculated. Assumes the presence of a temperature field called T.

If the numpy-library is found then global variables which are fields are being transformed to numpy-arrays. These arrays can be accessed with the usual numpy-array access like a[i,j] or a[i,:]. Global variables are made accessible by reference. This means that writing a value changes the global variable. Setting the whole variable has to be done by slicing a[:]=3 (a=3 removes it from the workspace). Vectors and tensors are two-dimensional arrays. They have convenience-attributes that return the whole vector of a component (like a.x for vectors or a.xx for tensors). To overwrite these they have to be sliced: a.x[:]=0 (a.x=0 only changes the attribute)

If a variable that is going to a global namespace is a numpy-array then it is translated by the following rules: vectors are transformed to scalarField. Arrays with 3 columns to vectorField, 9 columns to tensorField and 6 columns to symmTensorField. Different column-numbers produce errors

If this is set then this Python-code is executed every time a time-step was written to disk

Python-integration now has two convenience-functions that return a filename with the full path and create the directories if necessary. The file is not created (that is the responsibility of the Python-code).

The functions are (name is the name of the function object)

dataFile(fname)

creates a directory <case>/<name>_data/<time>. To be used for data that is written at times that differ from write-time

timeDataFile(fname)

creates a directory <case>/<time>/<name>_data. Should only be used for data that is written only at write-time

A command lione switch -noDimensionChecking is added that allows switching off the checking of dimensions if this makes expressions fail

If another case (with time and region) is specified via command line options (no dictionary) then in the expressions the other mesh can be accessed under the name other

Main application for this is comparing to other cases (but also comparing different timesteps of the same case with each other).

Used time is either fixed or set to the currently used (this can be selected via the command line)

Each expression can specify foreign meshes with a foreignMeshes-subdict

There are two new function objects:

addForeignMeshes

this allows specifying new foreign meshes. These can be used in subsequent function-objects or other swak-expressions on internalFields

foreignMeshesFollowTime

this allows specifying a list of meshes whose time is set to the current time of the running case

This helps debugging timestepping-strategies

A new possible entry for the accumulations calculates an average that is weighted by a facetor that depends on the entity:

• cell volume if applicable
• face area for surfaces etc
• $1$ if there is no appropriate weight (usually values defined on points). The result is equivalent to average.

The title says it all. Should give the user additional feedback about what is happening

This boundary allows specifying the partial slip fraction of the regular partialSlip-BC with an expression.

This is sometimes necessary to allow calculations with fields where the boundary conditions have a lot of dependencies (turbulence model, other mesh etc)

The option -additionalRegions allows selecting additional mesh regions for boundary conditions that require it (usually used together with -preloadFields).

For the other case there is an additional option -otherAdditionalRegions.

This option allows specifying additional field names to be preloaded in command line mode. If multiple mesh regions are specified (including another mesh)it will try to preload the field there too

Support for tensor-types has been added

For boundary conditions that require other fields these can be loaded into memory

The utility now allows the selection of timesteps. In that case it acts fundamentally different: instead of doing a timeloop it jumps to those times, calculates the boundary conditions and writes. The purpose of this mode is generating boundary fields for postprocessing.

As the majority of installation problems were actually problems with the compilation of the library swak4FoamParsers and as this library is central for all other things in swak4Foam the compilation terminates if this library is not built

This new header includes information about the swak4Foam-version, the OpenFOAM-version and macros for workarounds that depend on the OpenFOAM-version

This forces the entries to be checked while being read. Allowing more consistent treatment

This script allows compiling additional versions of swakPythonIntegration for cases where the version on the development machine is different from the version on the simulation machine (see installation chapter)

Changes without consequences for the user

The valid characters for an identifier were the same as in word (was string before)

The list of contributors to each file have been added (mostly by script with the information from the repository)

This abomination from the early days of funkySetFields has been cleaned

Changes to the documentation

A first version of a reference manual is added. Only the first part about expressions and parameters is written.

This is the first version to compile with OpenFOAM 2.2

Due to changes in OpenFOAM it requires several #ifdef (something that is usually avoided in the OpenFOAM-world) and other prepocessor definitions)

Due to incompatibilities between OpenFOAM 2.2 and previous versions there are compatibility headers included from the rest of swak4Foam.

Theoretically both libraries can be easily made independent again.

The last release (0.2.2) did not compile on 1.6-ext. This is fixed

Due to a stupid .hgignore the 0.orig-directories were missing. Nobody complained though

This has been fixed

With the options autoWriteSurface and autoWriteSets sampled surfaces and sets are automatically written at each write time. With writeSurfaceOnConstruction and writeSetOnConstruction both are written when they are created. A format has to be specified. No values are written.

These function and some other minor ones (sph, dev2, twoSymm) are now supported by the parsers

The component operators .x, .y and .z now extract the rows from a tensor

As this situation (like a variable named p for the position that shadows the pressure field p) leads to weird errors a warning is given. The warning can be switched of with the option variableNameIdenticalToField.

According to the convention introduced in OpenFOAM 2.2 now the data directories generated by functionObjects based on simpleFunctionObjects (that is almost all) and swakPythonIntegration (if the Python-code uses the dataFile-function) are generated as sub-directories of postProcessing in the case directory.

Scripts that rely on the location of these files will have to be adapted

This is due to a fix that now allows reading/writing these in binary mode. Only occurs if reading old data that either

• uses a delayed variable
• has global variables written in timesteps

This may break them for previous versions of OpenFOAM

The C-files generated by bison become very big and some compilers need quite long when aggressive optimization is used. An additional environment variable SWAK_COMPILE_GRAMMAR_OPTION allows the specification of additional compiler switches (like -O1) that will appear after the regular switches and should alter the behavior of the compiler. Set in swakConfiguration if you want to set this permanently

Some distributions don’t use good old bash as the default shell. This breaks some scripts in subtle and not so subtle ways

To filter bug-reports with outdated versions

Changes without consequences for the user

Methods that look for fields now use the appropriate data type

There were template specializations for pTraits in ExpressionResult.C that had to be moved to ExpressionResult.H to allow compilation on these non-=gcc=-compilers

Even if the condition evaluates to false the function objects in the list are executed. This makes the run fail if the purpose of the condition was to guard from such a situation. Fixed

This was fixed by writing the fields properly with writeValue. This may introduce a little incompatibility when reading files written by old versions

These fields were registered with the mesh which might have disturbed similar named real fields. Also did the fields generated for variables get registered

Missing initial conditions made this case a bit pointless

This was due to the boundaries being set to 0. Fixed. Also for the dist() function

The library simpleSearchableSurfaces adds more searchable surfaces to be used in snappyHexMesh. Types of surfaces in that library are

• some objects that duplicate existing surfaces and are only there for historical reasons (except the cylinder which distinguishes between different sides). Others wrap existing surfaces and expose the different sides
• wrappers for other surfaces that do coordinate transformations with it: rotation, translation, scaling
• wrappers that take two surfaces and do boolean operations with them: union, intersection, difference, exclusive difference
• Some wrappers that manipulate the regions of a surface: rename them, collect them into one region

This type is used to collect multiple values. If it is assigned a value then the uniform value of the right hand side is appended to the variable. Useful for collecting multiple values for output.

Variant StoredStackExpresionResult keeps the values between timesteps and allows the collection of timeline data

Dumps the value of a global variable into a line of a file

Removes a global variable (mainly used to preserve memory)

This dictionary allows the specification of alias names and their real names. If an alias name is found in an expression then it is replaced by the real name when looking for fields. The application for this is that OpenFOAM allows characters in field names that are not valid in swak-names and would break the grammar if they were (for instance - or :). By setting an alias such fields can still be accessed.

The function object listRegisteredObjects in the simpleFunctionObjects lists all the objects currently registered with the mesh. Mainly used for debugging (“Which fields are currently available?”)

The new functionObject executeIfParallelSerial allows specifying if a list of function objects should only be run if the simulation is running in serial or parallel.

There are now four function objects that calculate distributions of fields. Distributions are calculated based on the Distribution-class that is part of OpenFOAM starting from version 2.0 and uses a weighting for added values. There are two kinds of output

• a timeline with the key characteristics of the distribution
• directories with the distributions at specific times. These are written “raw” and accumulated

For tensors and vectors these are output separately for every component. These outputs can be switched on and off separately. The user has to specify the bin-width for the classification. If the bin-width is too small and the distribution becomes too small it is scaled down.

The two function-objects in the simpleFunctionObjects are:

fieldDistribution

distribution of field values weighted by the cell volume

patchFieldDistribution

distribution of a field on a number of patches weighted by the face area

In swakSimpleFunctionObjects the two functionObjects are:

swakExpressionDistribution

distribution of an expression on some entity. The user also has to specify and expression weight with the weight of each value and a logical expression mask. Values are only used if mask is true at the place

patchExpressionDistribution

distribution of expression on a number of patches. As the weight the face-area is used

This allows other variable types like stored variables to be inserted there. They are also now saved for restarting

All classes using the python interpreter now have a variable endTime with the current end-time value

If one of the functionObjects for time-manipulation set the end-time and it is reached and this is no time for output a complete output of the fields is forced

This includes the patchExpression-functionObject. The supplied list is now interpreted as a list of regular expressions and all patches that match are included and processed

An optional parameter outputControlMode now allows control on when the function object will be executed. Possible values are:

timestep

Every outputInterval timesteps the object will be executed. This is the default behaviour with an interval $1$

deltaT

Approximately every outputDeltaT times it will be executed. The nearest possible timestep is used

outputTime

Executed whenever a regular output is scheduled

Two enhancements

• the name of the independent variable no can be specified. This variable holds the value that is passed to the data entry as a uniform value
• data entry can now be integrated. This allows using it for instance for the injection rate in lagrangian models

The reason for the jump in the minor revision number is that with the introduction of the parser for lagrangian particles (cloud) the last white spot as far as major data structures in OpenFOAM is “explored”

Due to certain differences this version only compiles with the nextRelease-branch of 1.6-ext (from the git).Usually the failing parts can be fixed b commenting out the appropriate #define in Libraries/swak4FoamParsers/include/swak.H.

As this version is quite similar to 1.7 a lot of #ifdefs were introduced by this port leading to a possible unification with the 1.x-branch

The error messages where already quite verbose. But people didn’t understand them and asked the same questions over and over …

As there are going to be more cross-dependencies the simpleFunctionObjects now have to be part of swak. Changes to the compile-scripts reflect this.

The script writes the version it is used with to disk and at later compiles that this is the same (this makes sure that not a wrong version is used inadvertently to compile)

There are two macros defined that inside an object write the name of the class and the address of the object (if debug is enabled). This makes the output easier distinguishable from the output from other classes/objects. The two macros are:

Dbug

Writes the debug information only on the master processor

Pbug

Writes the output on all processors and for parallel runs prefixes the processor number

Both macros are to be used like regular streams and don’t have to be enclosed in if(debug){} (this is part of the macro)

With some compilers (Intel) and aggressive optimization the lexers (whose code is generated by flex) have uninitialized memory and segmentation faults. In these cases now an environment variable SWAK_COMPILE_LEXER_OPTION to set lower optimization for these compilers. For example:

export SWAK_COMPILE_LEXER_OPTION=-O0

After that recompile

For some machines race conditions with compiling the main library has been reported. The reason seems to be that some source files need headers generated while compiling the grammar. If due to the large number of simultaneous compilation processes the headers have not been generated when these files are compiled the compilation fails.

This effect could not be reproduced on the development machine (but that doesn’t mean that this doesn’t happen on some machines). Nevertheless for the libraries where this might be the case the number of compilation jobs is limited to the number grammars in the library.

Better solution to let the Allwmake-script generate the headers before the regular wmake starts.

Several minor additions that should make packaging easier

• Package version now gets the correct distro name (at least on Ubuntu)
• Packaging picks up the correct python-version (2.7 or 2.6 … does anyone use older?)
• Packaging process leaves the swakVersion.H alone

Important enhancements of the documentation in the Documentations-folder

The possible values of the common accumulations-lists are documented

The general options and the behavior of the Python-embedding are described

Because of report https://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=177 to be consistent with the nomenclature in the ‘regular’ function-objects.

This method has been added in 2.2.x and breaks the compilation of several function-objects

Fix developed by Bruno Santos

For some reason using SuSp gave unstable results for the PDE-functionObjects. Changed to Sp

Bug originally reported https://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=179 in. Reason was that the variable describing the type was not correctly set.

The entries codeEnd and codeExecute were not correctly read but instead the entry codeRead was read. Fixed

Reported as https://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=172

Only the field parser correctly found logical variables (although they were stored). Added a method to pick up the variables (the reason why this part was commented out is that there is no such thing as a volBoolField and that is what the regular mechanism expected)

Reported as https://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=176

In that case the driver was written before the surface was updated thus generating fields of size $0$. Now update is called at various places (to make sure it is called in any instance)

This accumulation was available but not implemented. Now implemented.

For non-scalar types it is calculated separately for each component

This was due to a logical error that was propagated through mindless copy/paste (only the Field-driver got it right). Fixed

Because it is not initialized from the superclass when the dictionary constructor is used. Fixed

Because the pointer is already set. Fixed

If the dictionary was read after the construction the aliases are not read. Fixed by moving this reading to the tables reading which is used in every time a dictionary is involved

Passed a value where a reference would have been needed. Fixed

Reason for this was a change of the interface of outputTime not being propagated to this function-object. Fixed

The Python-integration returned single scalars (and vectors) not as a single value but as a field of length $1$. This caused warnings that messed up the output. Fixed

These were not compiled by accident. Fixed

As reported in http://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=190 if a face-set or zone has faces on a processor boundary incorrect values were produced.

The reason was that boundary faces are treated like internal faces. Also do these faces exist on both processors. This is now fixed. If the face is on a regular boundary patch the value is used. If on a processor patch the value is only used if it is on the owner processor.

This addresses http://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=190

Subclasses of simpleFunction-objects are not guaranteed to be parallel-aware (for instance swakExpression can have problems with stored variables if the number of cells/faces changes) so the notImplemented can’t be removed for good.

The workaround is a rather verbose error message and the possibility to override notImplemented with a dictionary-switch

The functionObject executeIfOpenFOAMVersionBiggerEqual only executes if the OpenFOAM-version is bigger or equal to a specified version. The arguments majorVersion and minorVersion are required. If patchVersion is not specified it will match any version. A git version (.x) will match any patch-version

The function object executeIfStartTime executes its children if the current time is the startTime from the controlDict (which isn’t necessarily the first time step in a restarted case)

To be used on an existing field to set reasonable initial conditions

Named recalcPhi in the simpleFunctionObjects. Usually needed when some other functionObject manipulates velocity or density

Name correctThermo. Recalculates the thermophysical model. To be used after manipulating temperature etc

Recalculate enthalpy, sensible enthalpy or internal energy according to the current temperature. This allows making this consistent if the temperature has been manipulated.

For OpenFOAM after 2.2 these are replaced by one that recalculates the energy or enthalpy

The function object swakExpressionAverageDistribution calculates the average of one function (the expression) as a distribution over another (the abscissa). An example would be the average pressure in x-direction with abscissa being pos().x, expression being just p and the weight being vol(). The weight has to be a scalar. All other expressions can be any data-type

This utility prints some quantitative statistics about a specified field. Optionally these statistics can also be printed for patches, sets and zones. The data can be written to a CSV-file. Also the distributions of the field can be written.

This utility needs a dictionary and a specification of times. For each time it

• loads a list of fields specified in the dictionary
• executes a list of function objects specified in the dictionary
• executes python-scripts

The idea is that the function objects pass data to the python-scripts via global variables and the python-scripts do whatever they like

This utility allows setting new fields of a lagrangian cloud. Like funkySetFields it has two modes:

• Setting one field over the command line. This is triggered by the -field-option
• Using a dictionary to specify what is being set. In this mode more than one field and more than one cloud can be set. In this mode there is also the possibility to specify a new cloud. This mode expects variables in global namespaces. On of these variables is the position of the particles, for the other variables fields of the same name will be created. All the variables have to be of the same size. Data where corresponding particle position is outside the mesh is discarded

There is now an additional parser to calculate expressions on particles.

This parser is organized in a separate library libswakLagrangianParser that has to be loaded to use this parser.

Depending on whether the cloud in question is already in memory or on disk the data is handled differently:

• if the data is on disc then the basic properties of the cloud (particle positions etc) are used to initialize the class. Then all files in the folder of the cloud are read and made available as field names that are the same as the file-names. Characters in the file names that are not compatible with the parser are replaced and created as aliases. In this mode swak has no idea about the data except the name and the type
• if the cloud is in memory then a corresponding proxy object is sought. This proxy object knows which data the cloud has, what the type is and a short description. It makes the data available as fields.

  swak has by default proxy objects for most particle classes that come with OpenFOAM. For unsupported classes and adaptor library has to be written.

When a parser for a cloud is used for the first time a table of all the available fields is printed to the screen with type and description (if available)

If the field is found in memory this is used instead of a file read from disc.

An additional switch writeBeforeAfter allows writing the field before and after solving

Mode startup executes the FO only during construction

It is now possible to add a sub-dictionary else that is used to initialize a functionObjectProxy that is executed if the condition is not fulfilled. The sub-dictionary inherits all settings that are not set from the parent-dictionary

The entry codeData is now read and inserted into the functionObject

The two parsers in that library now also support the complete set of tensor operations (like eigenValues etc)

For expressions whose results is not a scalar now the weight function can either be a scalar or of the same type as the expression (so every component can have a separate weight)

A number of possible accumulations have been added. Most of these are based on distributions. If the weighted variant is chosen then the meaning is the more physical one (for weighted the ‘natural’ weight of the quantity is used. For instance for cells the cell volume. Otherwise the weight $1$ is used). Some of these accumulations need a single floating point number as a parameter. This is simply added to the name. The added accumulations are:

weightedSum

sum of the quantity times the weight. There is an alias integrate for this

median

The value for which 50% of the distribution are smaller than this. More robust alternative to average

quantile

quantile0.25 for instance is the value for which 25% of the distribution are smaller than it

range

The difference of the quantile of $\frac{1+f}{2}$ and $\frac{1-f}{2}$. For instance range0.9 gives the range in which 90% of the values are (from the quantile 5% to 95%)

smaller

The fraction of the distribution that is smaller than a given value

bigger

The inverse of smaller

size

The size of the underlying entity (usually number of cells, faces, points). For types with more than one components all the components have the same value

weightSum

Sum of the weights of the underlying entity. Usually the volume oder the area of it.

If a file specified with an option like startFile in a Python-functionObject (or similar) is not found in the current directory the path of the dictionary it is specified in is prepended and the file is searched there

The interactive shell of the python integration now uses IPython if it is installed. This improves tab-completion etc

As problematic libraries could hand during importing these libraries can be imported in a safe way using the optional importLibs-entry which is a dictionary. The keys are the names under which the imports will appear in the Python-namespace. The value is optional and the name of the actual library

All parsers now implement a function weight() that returns the “natural” weight that is used for instance in the weighted average (for internal fields that would be for instance the cell volume)

Two kinds of files are optionally written

• CSV-files with the values of an evaluation (each evaluation gets its own file)
• Distributions of the evaluations (in a separate directory for each time)

All the files go into a directory whose name is derived from the name of the evaluation. The outputs can be switched on with the options writeDistributions and writeCsv. Either

• from the command line: this switches it on for all evaluations
• one “per dictionary”-basis for each evaluation separately

The PDE-functionObjects now honor the relaxationFactors. If =steady is false then relaxation has to be switched on using relaxUnsteady. For the last corrector iteration the equation is not relaxed unless the parameter relaxLastIteration is set.

The support of laplacian operations (especially with a coefficient that is different from a scalar) was incomplete. Now all possible coefficient types are supported.

Also in the fvcSchemes-plugin functions the set of laplacian-operators was completed

If the logical expression mask is set then only the results from expression for which mask is true are used for accumulations

Started one new directory for all cases from presentations

Two new examples

sandPitsOfCarcoon

Reenacting a scene from “Return of the Jedi” with twoPhaseEulerFoam

landspeedersInCanyon

Simulating two landspeeders from “A new hope” with simpleFoam

There is now a new code-snipplet required for a number of these function objects. It can be left empty but has to be specified

The expressions used with swakExplicitSource, swakImplicitSource and swakSetValue now also need a dimension. This dimension is used to make sure that the user “knows” the actual dimensions of his source terms

This version adds support for OpenFOAM 2.3. The major changes were due to changes in the API to

• searchableSurface
• meshToMesh

And several minor adaptions

No major changes required. Runtime-selection tables are now sorted too

This should make swak.H more readable

If a directory privateRequirements/bin is private in the sources directory then the bison found there is used. A script maintainanceScripts/compileRequirements.sh is provided that fetches the bison sources, compiles them and installs them there

A section about thus new feature is added

The distribution data was not clipped to the range where actually data was collected. This is now fixed by adding the notion of an invalid value to SimpleDistribution

This should now be fixed

Because of the missing dimensions until now swakExplicitSource and swakImplicitSource were not actually working

Always set source etc for whole region. Now the selectionMode is honored (for instance only in cellZone the source term will be applied.)

Problem is that when the processor boundaries are used too that the indexing might be inconsistent on the different processors. Fix: coupled boundaries are ignored by default (have to be switched on)

In newer version the execute()-method of function objects needs a parameter force. Fixed

Due to a small semantic difference in the copy constructor of GeometricField a temporary object of the same name shadows the real field and prohibits that it is written. Fixed by giving the copy a unique name

These boundary conditions allow specifying a value in normal direction to the patch while in tangential direction the regular slip condition is applied. This is implemented for fvPatch and pointPatch. For the pointPatch the normal direction has to be specified by the user

Utility that calculates new point values for the mesh. In the simplest form the expression is specified on the command line. If the option -expression is missing the program looks for a dictionary which allows more control. If -relative is specified points are moved by the result of the expression. The result of the expression must be a pointVectorField

A hierarchy of function objects that trigger additional writes. Once a condition is fulfilled data is either written for a specified interval or as long as the condition is fulfilled. After that a cooldown period is possible. During this period nothing is written.

The concrete function objects are

writeIfFieldOutside

writing is triggered if the minimum or

the maximum of a field is outside a specified range. Part of the simpleFunctionObjects

writeIfSwakExpression

writing is triggered if a logical expression evaluates to true. Stopping and retriggering is also possible with logical expressions. Part of the simpleSwakFunctionObjects

writeIfPython

writing is triggered by a Python-snipplet that either returns True or False. Stopping and retriggering are also possible. Part of swakPythonIntegration

Allows saving and writing a specifiable number of timesteps before the condition is met (this allows finding out what lead to this)

This function object installs a new signal handler for specified signals.

The function object itself saves the last $N$-timesteps, the signal handler (when called) writes these steps to disk and then calls the regular OpenFOAM signal handler

Starting with OpenFOAM 2.2 (where the concept of fvOptions was introduced) there is an additional library swakFvOptions with special fvOptions (in addition to those in swakSourceFields):

executeFunctionObjectsFvOption

this one does not manipulate the fields (as expected) but “only” runs a list of function objects. Application is for instance to get information during the time-step for algorithms that have multiple iterations in a time-step

reportAvailableFvOptions

Does no manipulation of the solution/equations. Simply reports that a callback has been called. Application: find out which fvOption-calls are used by a solver in which order without going through the sources

reportMatrix

Does not manipulate the matrix but prints a number of metrics

For expressions and variable lists there is now the possibility to expand values from the dictionary during reading. The two characters that trigger this are

$

like the regular variable lookup in OpenFOAM.In its most complex form it looks like this $[(type)spec] where spec specifies where to look for the value (including scoping if the OpenFOAM-version supports it). The optional type specifies how the entry should be interpreted

#

in variable lists: #otherList; includes the variable list otherList instead of this entry

These expansions allow the construction of reusable snipplets that include information from other parts of the case. For instance (this is only part of the specification)

#include "$FOAM_CASE/constant/g"
vecName U;
downComponent (
    "grav=$[(dimensionedVector)g];"
    "down=($vecName & grav)/mag(grav);"
);
variables (
    "#downComponent;"
    "maxDown=max(mag(down));"
);

would calculate the component of a vector field that points in the direction of the gravity (as specified in the g-file).

This expansion is done during the expression.

An optional entry dimension for the function object now allows setting the dimension of the resulting field

This function gives the distance in the mesh to a specified face.

Not yet working correctly

With the switch storeAndWritePreviousState this functionObject now can cache a number of timesteps and write these results in addition to the current timestep

In addition to the average now this Function object also records the minimum and maximum value for each bin. Also the number of samples used in the bin

The function objects executeIfPython, setDeltaTWithPython, setEntTimeWithPython and writeAndEndWithPython now expect code snipplet named init. This is executed in the beginning and can be used to set up global variables if these snipplets need some kind of state. The variables have to be declared global in the snipplets that do the actual decision (for technical reason)

The function objects solveTransportPDE and solveLaplacianPDE now call the regular fvOptions-callbacks (this allows modifying the solution in the same way it can be modified for solvers)

Example to demonstrate funkyWarpMesh and post-processing on bended geometries

This is the last release to support OpenFOAM 1.7.x and older

These are things that will happen in the next release and will break backwards-compatibility

As version 1.7 is several years old this release will be the last release that supports it.

Starting with this release the port_2.x-branch will become the default branch and the 1.x will become legacy

Due to the umber of different supported Foam-versions not all the examples run on all versions and it is not possible to fix them in such a way that they work on all versions. In the next version they will by adapted to use the pyFoamPrepareCase.py utility as this supports having different Foam versions in one case. As a consequence most cases won’t run without an installed PyFoam

If value is unset then during initialization the value of the internal field next to the patch is used. Previous behavior was to set the patch to $0$.

In most cases the new behavior should be better.

As OpenFOAM does not support geometric fields of type boolean swak uses scalar fields for storing truth values (only in the internalField-parser). The semantics was that a value of 0 means false. Everything else true. Logical operators set true to $1$ and false to $0$. As the test for equality to $0$ may sometimes fail this semantics is changed slightly: values $&gt;\frac{1}{2}$ are interpreted as true. All others as false.

If operators were used properly this should not matter, but expressions that assume for instance that 0.1 is true will now fail. Overall this change improves the stability of logival expressions

The improved detection of single values might break some expressions. Especially for the Python-integration as values that were previously passed as arrays are now being passed as single values

This reflects a change in the API of the kinematic lagrangian parcels. The old function has been discontinued to avoid confusions with changed semantics

For parallel runs this signal is now automatically switched in so that other signals are propagated to other processors

Due to a different calculation automatically calculated bin-widths in this function object might slightly differ from previous calculations

For the swak-function objects the data is now written to a directory whose name is based on the input dictionary instead of postProcessing.

This might break scripts and other post-processing procedures that rely on the data being in postProcessing.

Data generated during the run-time of the solver is unaffected

Only minor adaptions. Mainly to accommodate the new debug switches

Compiles with OpenFOAM 2.4.0 (and 2.4.x)

Results that were booleans used to report bool as their type for the internalField-parser. Now they report volLogicalField, surfaceLogicalField or pointLogicalField. This makes them consistent with the possibility of requesting these start symbols and specifying logical fields in the parameters of a plugin function

If the span of the abscissa is too small (almost $0$) there were numeric problems. In this case the bin-width is now extended to $1$

Reason was that SimpleDistribution.calcScalarWeight did not reduce. This is now fixed (and a special switch is introduced for one situation where this isn’t desirable)

On OpenFOAM-versions with fvOptions these were broken because of inconsistent dimensions.

This is fixed: now if a fvOption is defined the function-objects also needs rho and this is passed to the call of fvOption when generating the source term

As reported in https://sourceforge.net/p/openfoam-extend/ticketsswak4foam/225/

Problem seems to be that the HashPtrTable is not correctly read in binary-mode. Workaround is to switch to ascii before writing and reading that table and then switch back to the original mode

Single values like min(expr) were passed as arrays instead of a single value. This is now fixed. The problem is that now expressions that rely on the old behavior might break

If all data falls into one bin of the distribution then the distribution was not written. This is now fixed

Fixed

If the current time was already written (because it is part of the stored times) a segmentation fault occurred. This has been fixed by checking whether the current time is already stored

This has been fixed

The scripts

• makeSwakVersionFile.py
• makeCopyrightEntries.py

have been adapted so that they now work with Python 2.x as well as Python 3

This function for the field parser gives the distance in the mesh to a specified patch. Distance is defined as minimial sum of cell-to-face distances needed to reach this cell from the named patch

If a SIGSEGV or SIGFPE were encountered only on some processors then on the others no data was written because these signals do not propagate to other processors

Now the signal handler raises a SIGTERM which is propagated to the other processors. For parallel runs a signal handler for SIGTERM is automatically set up to make sure that on all remaining processors data is written

Provided by Alexey Matveichev

The script maintainanceScripts/make-releases.sh rolls a release and puts it into the directory releases

Provided by Alexey Matveichev

Automatically finds the linking options for Python with python-config

Similar to distToPatch there are now two additional built-in functions:

distToCells

A logical field is provided. The distance to the cells for which this field is true is calculated

distToFaces

Same as distToCells but with a logical function for the faces

Both functions return cell-values

This library collects functions that are similar to distFromPath: they use the MeshWave-algorithm to calculate distances and connectivity of the mesh.

Functions in this plugin are:

meshLayersFromPatch

Calculates for each cell how many mesh layers it is away from a patch

meshLayersFromCells

Calculates the number of layers from a set of cells selected by a logical expression

meshLayersFromFaces

Calculates the number of layers from a set of faces selected by a logical expression

floodFillFromCells

Number connected regions. Cells selected by a logical expression separate these regions

floodFillFromFaces

Number connected regions. Faces selected by a logical expression separate these regions

cellColouring

“Colors” the cells in such a way that no two neighboring cells have the same number. Mainly for visualizing the mesh structure. “Neighboring” means “cells sharing a face” not an edge. Therefor it may look at the surface like there are cells with the same color

Additional functions:

mqCellFaceNr

Number of faces for each cell

mqCellShape

Field with numbers describing the cell shape. Values are:

1

Hex

2

Prism

3

Wedge

4

Pyramid

5

Tetraeder wedge

6

Tetraeder

0

no classification. Polygon

The function object provokeSignal can be used to debug signal handling. No other possible use is known.

The function object allows defining the signal, the time and - in case of parallel runs - the processors on which the signal should be raised

This function object executes a lost of function objects if face/cell/point sets or zones are present. The required zones and sets are specified in a dictionary setsAndZones: keys are the names of the entities the values are the types (like faceZone). Only if all objects specified there are present the function objects are executed.

As a side effect if loadAndCacheMissingSets is true than sets that are not yet found in memory are loaded from disk. Attention: if no set of that name is found on disk then it is searched at every time-step. This is a potential performance problem (it is not a problem if the set is there)

This function object executes a lost of function objects if a list of patches is present.

This function object shows data that is stored in the mesh. Mostly solverPerformance with the residuals of the linear solvers

This function object gets a list of fieldNames and gets the information about their solver performances. The three quantities that it gets are

nIterations

the number of iterations

initialResidual

residual before iterating

finalResidual

residual after iterating

For each value three variables are created (assuming the field is named foo):

foo_nIterations

array with all the values. This is usually only usable in the Python-integration

foo_nIterations_first

value of the first solver performance

foo_nIterations_last

value of the first solver performance

simpleFunctionObjects now has a base class that allows manipulating fvSolution and fvSchemes in-memory but the solver behaves as if the file changed on disk. Application for this is changing parameters like relaxation or discretization schemes during the simulation. This can be used for instance to start the simulation with ‘safe’ settings and switch to faster convergence later.

There is currently only one function object timeDependentFvSolutionFvSchemes that implements this (more are planned). It allows switching to different subdictionaries at specified time. An example can be found at Examples/manipulateFvSolutionFvSchemes/pitzDailyTimeSwitched. This function object gets a list of times and sub-dictionaries. At the specified time the values from the sub-dictionary overrides the values in the original dictionary (Values not present in the sub-dictionary are left untouched). If reset is specified as the name for the sub-dictionary then the dictionary is set back to the original state.

Until no if value was not set groovyBC automatically initialized the boundary to $0$ until the actual expressions were evaluated for the first time. This raised problems when people for instance didn’t initialize T to $0$ and the density calculation produced a division by zero.

Now if value is unset then the value of the patch is initialized from the value of the internal field next to the patch. This doesn’t protect from the internal field being

With an additional optional argument cloudNames a list of clouds to be written can be specified like the fields.

This feature was implemented by E. David Huckaby

For utilities for which this is appropriate this allows loading function plugins from the command line (without adding them to the libs-entry in the controlDict). It is assumed that the name of the library starts with libswak and ends with FunctionPlugin.so.

If a list of words named functionPlugins is found then the string libswak is added in front and FunctionPlugin.so is added at the end and a library of that name is loaded to add the functions provided there

Now it is possible to handle SIGUSR1, SIGUSR2 and SIGTERM. Only needed for testing

If a code is a string of the length $0$ nothing is done. This is especially important as no global namespaces are read (which may not be created at the time. Especially during initialization)

If a dictionary specifies the entries mask and weight then these are evaluated and used to mask and weight the data specified in expression

If specified in the sub-dictionary the entries distributionMaxBinNr and distributionBinWidth allow setting the number of bins. These values are not used exactly but give the distribution class a hint. distributionMaxBinNr takes precedence

For parallel runs the process that initiates the writing of data waits for the other processes to write their data. This time can be specified with a parameter sleepSecondsBeforeReraising that has a default value 60

The function objects based on writeAndEnd now have an optional switch storeAndWritePreviousState. If this is set then a number of old time-steps can be stored and will be written when the run is terminated.

In 2.3.1 two new forms of addSup where added to fvOption (one for compressible equations. The other one for multi-phase solvers). Both new forms are supported by all fvOption-subclasses in swakSourceFields and swakFvOptions

When the switch dynamicExtremesAbscissa is false then the limits of the distribution can be set with minAbscissa and maxAbscissa. This mainly influences the bin-width. If values fall outside this range then the distribution is extended to accommodate these values

This involves almost all function objects in swak that write data to postProcessing. The library now allows setting a different default. This value can also be set with an optional entry postProcDir on a per-function-object basis.

This change is used in the funkyPythonPostProc-utility to set a directory name that is based on the name of the input dictionary (or set with an option). Now if there are function objects used they will write their data to this directory instead of postProcessing (leaving data generated during the running of the solver alone)

Note: This only works for function objects from swak. “Regular” function objects will still write to postProcessing

An additional option -correctResultBoundaryFields corrects the boundary conditions before writing to disk. In dictionary mode there is also an option correctResultBoundaryFields.

This is only needed in rare cases.

This case demonstrates how to add lagrangian particles to the simplest tutorial-case

This is the first release that does not support OpenFOAM 1.7.x, OpenFOAM 1.6-ext and older versions anymore

This version adds support for OpenFOAM-dev published at git://github.com/OpenFOAM/OpenFOAM-dev.git

As this version is constantly changing it might or might not work with the most up-to-date version of the repository.

The port is maintained in a branch feature/port_of-dev that is never closed and is periodically merged to the develop-branch.

Internally the dev-version is maintained as version 9.9.99

Support for this version has been added (basically all the fixes from the dev-branch were guarded with the correct version

Fields that have names that are not considered proper variable names by swak (because for instance the have a dot in the name like alpha.water) were not handled by fieldReport. This has been fixed

The reason is the initialization with pTraits::max and that during the calculation of mag this causes an overlflow. Fixed by scaling down to the square root of the maximum

Because of this compilation in 2.2 failed. Fix provided by Bruno Santos

The reason was that the solverPerformance-class is hidden in lduMatrix. Fix provided by Bruno Santos

For OF-versions where fluidThermo and solidThermo have the same base functions like thermo_Cp can be used for solids too

Because of a bug in the lexer lookup tables did not work. Fixed

The macro that guarded the code needed for some OpenFOAM-versions did not include OpenFOAM 3.0. Fixed

The wrong flags were checked and the function objects were always executed when even if doMakeAbsolute and doMakeRelative were set to false. Fixed

A reference to a label that was passed to a flex-function broke compilation because that expects a 32-bit integer. Fixed

New version of org-mode makes changes in the UML-code necessary

Like the optional list lookuptables it is now possible to have a list lookuptables2D with 2-dimensional lookup tables. A table with the name tbl can be used like this in expressions: tbl(expr1,expr2). expr1 and expr2 must evaluate to scalar values of the same entity (cells, faces, points …) and the expression will evaluate to a scalar.

This feature is based on the interpolation2DTable that is part of OpenFOAM since 2.2 but there is a modified version of this class included in swak4Foam as there is a problem with the output in the original version. Currently foam-extend is not supported as this is missing some base classes as well (tableReader)

These functions from fvc were implemented as plugin-functions. Mainly to be able to test their behavior. To check what they do see fvcSmooth.H in finiteVolume

Functions from the public interface of basicThermo and turbulenceModel have been added (like kappa, kappaEff etc)